Associative measurement of flat pattern perimeter and area 2

[SiW979]

Hello All

A bit of a long shot, but worth an ask. Our manufactuing eningeers have asked if it is possible for us to put the total perimeter and area of each of our sheet metal flat patterns on the drawings. I know we can use the measurement tools and area using curves etc, but this isn't ideal as it is fairly labour intensive. Therefore I was wondering if there might be journal ( oh hello Cowski) floating about that I could assign to a button that could out put this information either as an attribute or associative measurement that I could then add in to our drawing border. All our flat patterns live on layer 131 and are coloured pure blue.

Thanks in advance

Si

Best regards

Simon NX7.5.4.4 MP8 - TC 8

http://www.jcb.com

 

[cowski]

Do you have a flat solid in the file? If so, you may be able to create an associative face measurement that gives what you want by using the tangent face rule.

www.nxjournaling.com

 

[SiW979]

Tried that Cowski, it measures the perimeter of every face edge not just the out line so the out come is wrong, e.g. I just measured a plate using measure face, it reported a perimeter of 1756mm however is I manually measured the outline, it reported 1421mm :-(

I guess KF would be the way forward with this.

cheers

Si


Best regards

Simon NX7.5.4.4 MP8 - TC 8

http://www.jcb.com

 

[JohnRBaker]

Well, I have a really elegant solution, unfortunately while technically this should work in NX 7.5 we're aware of a limitation in creating Associative Measurements on models which are later updated. The good news is that issue was resolved in NX 8.5 so I'll outline the procedure so that people understand how they could make this work when and if they upgrade to NX 8.5.

What you do is to first create a new master template part file for use when creating Sheet Metal models. In this template file create a default 'Tab' feature (the size is not critical). Now create a 'Flat Solid' feature from this Tab and place it on some invisible Layer, but before you do that, using...

Analysis -> Measure face...

...with the 'Face Rule' set to 'Tangent Faces' and the 'Associative' option toggled ON, select the same face that you selected as the 'Stationary Face' when created the 'Flat Solid' feature. This will result in Area and Permimeter Expressions being created. Then create a pair of Attributes which reference these values. Now save this part and in the future use it as your template or 'start part' for when creating Sheet Metal models. You simply edit the default tab to whatever your desired size and then go from there adding tabs and other Sheet Metal features. Since the 'Flat Solid' is always the LAST feature in the tree and since the 'Measure Face' feature is after the Flat Solid feature it will update as features are added to the model (this is the problem which was addressed in NX 8.5 where the Associative Measurement results were NOT honoring the 'Face Rules' when additional faces were being added to a model).

Anyway, for those of you who are on NX 8.5, if you would like to give this a try, I've attached an example of what this template file would look like.


John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
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To an Engineer, the glass is twice as big as it needs to be.

 

[cowski]

The model you measured, does it have any internal cutouts?

I think a journal can be made to do what you want; unfortunately, I don't have that journal lying about at the moment.

www.nxjournaling.com

 

[SiW979]

Cowski

The vast majority of our sheet metal parts have cut outs in them of some description.

Best regards

Simon NX7.5.4.4 MP8 - TC 8

http://www.jcb.com

 

[cowski]

Do you want the internal cutouts included in your perimeter calculation or should they be ignored (only outside perimeter is important)?

www.nxjournaling.com

 

[SiW979]

Cowski

All cut edges are important as they will use the manufacturing guys will use the infomration on the drawing for time/cost planning.

Cheers

Si

Best regards

Simon NX7.5.4.4 MP8 - TC 8

http://www.jcb.com

 

[cowski]

Is John's method going to work for you?
If not, what needs to be done differently?

www.nxjournaling.com

 

[JohnRBaker]

My approach is only valid for NX 8.5, for a couple of reasons.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[SiW979]

I tried Johns method and as he quite rightly states it doesn't work in 7.5. I don't think it is possible with any of the tools I have at the moment, I was looking at trying to create a section through the mid plane of the flat solid and using section curves, but basically I just need to be able to uise the 2D curves of the flat pattern to get area of a face and combined lengths of all the perimeter of all cuts be they internal or external, it can be done using a area using curves and but I was hoping for something slicker.

Cheers

Si

Best regards

Simon NX7.5.4.4 MP8 - TC 8

http://www.jcb.com

 

[cowski]

After some experimenting, I think there is a viable (though not elegant) workaround for 7.5.
[ol 1]
[li]Create a flat solid[/li]
[li]switch to modeling, extract a face (tangent faces option) from the flat solid[/li]
[li]use the join face command on the extracted face (on same surface option)[/li]
[/ol]
This gives a single face that you can use for the associative face measure command. In the (admittedly simple) file I was working with it updated properly after changes were made (flanges added, cutouts added, etc).

www.nxjournaling.com

 

[SiW979]

Thanks Jeff, but I think I will wait until the summer and 8.5. I'll tell the manuf' guys it's not possible at the moment.

BTW...

How do you reference expressions in an attribute that you can then place on a drawing? Say for example I create an associative face measurement, how do I pull the parameters in to an attribute?

Cheers

Si

Best regards

Simon NX7.5.4.4 MP8 - TC 8

http://www.jcb.com

 

[cowski]

How to pull a face measurement to an attribute (NX 7.5):
Let's assume the measurement we want to assign to an attribute is expression p1; we'll need a name for a part attribute to hold the measurement value (I'll call it MEASURE) and an expression that will assign the value of p1 to MEASURE (I'll call it M1). Of course the names can be whatever you like.
[ol 1]
[li]In the expression editor, create a user expression (M1).[/li]
[li]For M1's formula enter: ug_setPartAttrValue( "MEASURE", format("%f";p1) )[/li]
[/ol]

The part attribute may not automatically update when the part changes. If it doesn't you'll need to execute the command update for external change (in the tools menu).

NX8 or higher will make this process much easier. It has tools to directly assign an expression value to an attribute (or vice versa) and the updating is taken care of automatically.

www.nxjournaling.com

 

[JohnRBaker]

Starting with NX 8.0 you can now create Attributes linked directly to Expressions, and vice-versa, WITHOUT having to use the KF functions provided in the Expression system 'Function' library which was the method prior the the release of NX 8.0. Of course you can always just create a Drafting note linked to the Expression, but in Master Model mode that would require passing interpart expressions where as the Attributes can automatically be inherited by the 'Component' in the Master Model Drawing file where they will then be referenced by a Drafting note.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[SiW979]

John

I have now got NX8.5 however your method doesn't take into account jsut the outside loop of curves, it will measure every single face edge. so when I put a flange on the tab the perimeter is 4 combined edge lengther more than is required. Am I missing a trick.

Si

Best regards

Simon NX 7.5.4.4 MP8 and NX 8.5 (native) - TC 8

http://www.jcb.com

 

[cowski]

The problem is you have multiple joined faces when what you need is one face.

I think my workaround posted on 8 Jan 13 11:05 would take care of your problem. You might even be able to skip the extract face step and just perform a "join face" on the flat solid then take the measurment from the resulting single face of interest (untested).

www.nxjournaling.com

 

[JohnRBaker]

Yes, you would need to perform a 'Join Face' on the final flat-solid, after which the Measurement would now be correct (and I did test this with NX 8.5). And once done, any additional flanges added to the Sheet Metal model will cause the flat-solid to update as well as the Join Face operation, which means that the 'Perimeter' measurement will remain up-to-date since by definition the new Sheet Metal features will always be added PRIOR to the Flat-Solid feature after which the Join Face and the Measurement will then update. A bit elegant, but usable.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[SiW979]

On the subject of flat patterns, if there is not already a plan to do so would it be worth raising an ER to allow the user to time stamp the flat patter so that it allows features such as chamfers to appear after the flat pattern. We add lots of weld preps to our heavy gauge plate and where these chamfers go over bends in the material, it causes havoc with the flat pattern and we have to resort to WAVE linking the model at time stamp in the MM drawing in order to omit the weld prep features. A right royal pain in the @ss. Have a look at the attached flat patterin the attached part, look specifically at the hole in the middle of the flat pattern. Fail :-(

Cheers
Si



Best regards

Simon NX 7.5.4.4 MP8 and NX 8.5 (native) - TC 8 www.jcb.com

 

[JohnRBaker]

Yes, open an ER to allow a user to explicitly, on a case-by-case basis, make the flat pattern/flat-solid feature either timestamp fixed or floating (as it does now).

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.